Inventor 101

[JD Mather]

 

Add a Horizontal constraint to the angled line and then change to Construction linetype.

 

Drag a corner of the rectangle - notice that is stays symmetrical top-to-bottom about the origin. Creating symmetrical relations like this is the key to Inventor sketching.

 

Exit sketch and save the file as Punch Base.

[JD Mather]

 

Dimension as shown.

 

TIP: DO NOT dimension to line endpoints (except at the origin) as lines can be trimmed and the endpoints you selected disappear. Dimension from line-to-line rather than endpoint-to-endpoint. This is the key to sketch dimensioning.

[JD Mather]

https://chronicle.autodesk.com/Main/Details/23894054-c11c-4f0b-9005-85c891bd69cb

 

Let's go pro.

Click on the link above and watch the video.

You can go directly into the arc command while in the line command.

Click and drag from the endpoint of a line (while in the line command) in the direction you want to go.

Then dimension the arc size and location and finally, drag the center of the arc to the construction line.

[JD Mather]

 

Extrude the sketch a distance of 30mm with a Taper of -7°.

[JD Mather]

 

Add 15mm Chamfers to the two outside vertical edges on the left side and 40mm Chamfers to the two vertical edges on the right side.

[JD Mather]

 

Add 30mm Fillets to the vertical edges of the two 40mm Chamfers.

[JD Mather]

Add a 15mm Chamfer all the way around the top outside edges (be sure to click the top of the previous 15mm Chamfers).

[JD Mather]

 

Expand Extrusion1 and turn on the Visibility of Sketch1.

Right click on Sketch1 and uncheck the Dimension Visibility.

 

Start a New Sketch on the top face of the part.

[JD Mather]

 

Project Geometry the centerpoint of the arc from Sketch1 as shown into Sketch2.

Sketch the Rectangle shown.

[JD Mather]

 

Add a Coincident Constraint between the projected center point and the midpoint of the left vertical line of the rectangle.

[JD Mather]

 

Window select the rectangle and toggle the line endpoints to Center Points.

 

Right click on Sketch1 and turn off the Visibility of Sketch1.

Finish Sketch2 and save the file.

[JD Mather]

 

Dimension the rectangle as shown.

 

We have two extra Center Points (at the midpoint of the left vertical line and at the projected origin) that we don't really need and could toggle to Points, but there is no real need to do this.

[JD Mather]

 

Start the Hole command and hold the Ctrl key and unselect the two extra points as shown. Enter 18.5mm Through All as the parameters.

 

(Tip: If you missed this step and accidentally created the two extra holes - you could always right click to edit the feature and then Ctrl unselect the two extra centerpoints.)

[JD Mather]

 

Turn the part over so that you are looking at the bottom.

Start the Shell command and click the bottom face of the part.

Set the Thickness to 10mm.

[JD Mather]

Oops, I forgot a step. Delete the file and start over - right? NO!

Well the step I "forgot" should have been done before the Shell feature. Delete the Shell feature - right? NO!

 

 

Find the red End of Part marker (hereafter referred to as EOP) in the browser and drag it up above the Shell feature.

[JD Mather]

 

Start the Hole command and this time use the On Point placement option.

Click the Origin Center Point for the Point and the bottom face of the part to set the Direction.

 

Click the Counterbored Hole option and set the parameters as shown.

 

Drag the red EOP back down below the Shell feature.

[JD Mather]

 

Turn the part over and start a new sketch on the top face.

Project Geometry the 4 edges as shown.

[JD Mather]

 

Sketch a circle from the hole center to the green snap point as indicated.

[JD Mather]

 

Trim the circle and then Extrude 8mm.

[JD Mather]

 

Add an 8mm fillet around the top edge of the extruded cylindrical feature.